Is there something I missed? I am getting this error in all the things I done. But a friend did one in his PC And I checked it in mine it worked.

emreg

November 13, 2011 06:39

hi,

i hav faced same problem last days.
i found that this is a mesh problem not an fluent settings error.

Follow this, if you will be succeed, inform me plz:

- Keep in mind that this error occurs usually while subtracting volumes.
Do u have some substracted volumes whic u performed in gambit?
Be careful while subtracting them especially for the volumes which they hav interfaces. (do u hav any interface BCs? )

- Check ur mesh and observe if there exists an error about Contact points.. exist?

inform me ...
regards,
emre gungor

tsram90

November 13, 2011 13:40

First of all. I don't have any subtracted volumes. ( I don't have volumes. Its 2D) Still I haven't done any face subtractions.

I don't have any interface BC either. Just 2 Vel in, 1 Pre out and rest are walls.

My geometry is quite simple. Just a square(defined using lines) with 3 valves in top.(also just lines)

I havn't got any error so far on contact points. I am not sure what they are and where to look for them. My grid-> check didn't give any errors

raj.cfd

November 14, 2011 12:39

Hi,

Negative volumes appear, if the centroid of a cell ( 2D or 3D ) is beyond the geometrical boundaries. Try getting a good mesh before proceeding further..

tsram90

November 14, 2011 22:17

Quote:

Originally Posted by raj.cfd
(Post 332054)

Hi,

Negative volumes appear, if the centroid of a cell ( 2D or 3D ) is beyond the geometrical boundaries. Try getting a good mesh before proceeding further..

Centroid of the 'cell is beyond cell boundary right. Not the total centroid?

How to get a good mesh? I am doing 2D so I tried meshs with equal interval size on all edges and both tri and quad meshs. The geometry is simple.Its a square.

raj.cfd

November 16, 2011 19:09

Hi,

From your original post, I can make out you are simulating a 2D IC engine - using dynamic mesh, right...??? . I have already worked on dynamic mesh for a IC-Cylinder. Here in your case , I suppose the negative volumes appear when the mesh is deforming/layer compression, ie when the piston moves from BDC to TDC. In order to solve this say for example, you have a piston, cylinder, bowl region, ports . you can create a pure quad mesh from the piston until the construction plane/reference plane and then upwards you can mesh it with tria. The construction plane is something like a reference plane until where the reciprocating motion of the piston takes place using dynamic mesh in FLUENT. You can either use smoothing, layering and/or remeshing option .You can probably look into IC engine simulation tutorial provided by Ansys Fluent. This should solve your problem.

tsram90

November 17, 2011 11:43

Quote:

Originally Posted by raj.cfd
(Post 332420)

Hi,

I suppose the negative volumes appear when the mesh is deforming/layer compression, ie when the piston moves from BDC to TDC. In order to solve this say for example, you have a piston, cylinder, bowl region, ports . you can create a pure quad mesh from the piston until the construction plane/reference plane and then upwards you can mesh it with tria. The construction plane is something like a reference plane until where the reciprocating motion of the piston takes place using dynamic mesh in FLUENT. You can either use smoothing, layering and/or remeshing option .

I tried starting from BDC and from TDC. I am getting negetive volume either way.( if from TDC then during down stroke.). I also tried reducing teh problem. Removed all vcalves, ports etc. Just a square. Still I am getting it.

I tried with Tri mesh only and quad mesh only. Getting error. I want to try using both of them mixed as said above. But I can't get any tuts on how to do it. Plz explain or give a link.

TQ..

karthickeyan

November 30, 2011 07:58

hi

hi friend
after seeing your post i found that you are using IN-cylinder motion. in that you are using remeshing ?because it only cause negative volume in dynamic mesh. you should give minimum cell size and maximum cell size value in remeshing option . it should be (0.4 *average cell size)and (1.2*average cell size)for maximum cell size. sorry for the delay in replying.

tsram90

November 30, 2011 12:06

Quote:

Originally Posted by karthickeyan
(Post 334110)

hi friend
after seeing your post i found that you are using IN-cylinder motion. in that you are using remeshing ?because it only cause negative volume in dynamic mesh. you should give minimum cell size and maximum cell size value in remeshing option . it should be (0.4 *average cell size)and (1.2*average cell size)for maximum cell size. sorry for the delay in replying.

TQ for the reply. I was seriously held back in with my project progress by this problem.

I am not using layering. using both Smoothing and remeshing.
I gave the values from the 'mesh scale info' just under where we give these value.

By ur method, how do we get the average cell size?

tsram90

November 30, 2011 12:55

Got It.

Adjusted the remeshing cell size in the Zone defining section with .4 and 1.4 of the avg cell length. (got length as min+max /2)

while specifying side wall as deforming there is an option 'mesh scale info' from that there is minimum cell size and maximum cell size from this take an average value and multiply with .4 for minimum cell size and specify for remeshing similarly 1.2 * avg cell value for maxicell value

famon

November 22, 2014 11:41

Quote:

Originally Posted by tsram90
(Post 334161)

Got It.

Adjusted the remeshing cell size in the Zone defining section with .4 and 1.4 of the avg cell length. (got length as min+max /2)

hi
when I enter following command (define/models/dynamic-mesh-controls)
after pressing enter it says :
invalid command [define]
could you please guide?

tsram90

November 22, 2014 12:57

Quote:

Originally Posted by famon
(Post 520518)

hi
when I enter following command (define/models/dynamic-mesh-controls)
after pressing enter it says :
invalid command [define]
could you please guide?

You have to enter it one by one..
define
models
...
...

famon

November 22, 2014 13:05

Thanks for your quick reply, worked ;-)

sanjeetlimbu

April 6, 2015 15:59

4 Attachment(s)

I am trying to simulate the compression stroke using 2D planner, mesh . I have to use axisymmetric option for my consider the real cylinder volume.
I made UDF and profile both case for the velocity of the piston. The inside will be gas mixture that I will load in chemkin import
I am unable to use the preview motion in both cases. I saw the piston with the profile - motion is as per the need, it move same distance I need. But it seems that the dynamic mesh is not good and causes the error

I am using Quad currently. Can u suggest the type of element to use for mesh and how to improve skewness /Orthogonal quality for the mesh to be used for the 2D axisymmetric case to represent the Cylinder

tsram90

April 7, 2015 02:56

Share your UDF and engine dimensions. Most probably the pistion is not returning, or you haven't given clearance volume.

Quote:

Originally Posted by sanjeetlimbu
(Post 540200)

I am trying to simulate the compression stroke using 2D planner, mesh . I have to use axisymmetric option for my consider the real cylinder volume.
I made UDF and profile both case for the velocity of the piston. The inside will be gas mixture that I will load in chemkin import
I am unable to use the preview motion in both cases. I saw the piston with the profile - motion is as per the need, it move same distance I need. But it seems that the dynamic mesh is not good and causes the error

I am using Quad currently. Can u suggest the type of element to use for mesh and how to improve skewness /Orthogonal quality for the mesh to be used for the 2D axisymmetric case to represent the Cylinder